# Confuse about Nu Number in Laminar Flow

 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 30, 2014, 08:40 Confuse about Nu Number in Laminar Flow #1 Senior Member   Join Date: Jan 2011 Posts: 272 Rep Power: 9 Sponsored Links Hi I did simple heat transfer problem of flow throw a circular pipe with constant heat flux at wall. Usually for laminar flow with constant heat flux the Nusselt Number should be 4.36 ? when I view surface nusselt number from Report>Wall Fluxes>Surface Nusselt number it give me Nusslet number as 11.61 ? Why this deffer from the theortical value as (4.36)? Mariam

 January 30, 2014, 08:54 #2 New Member   Smith Join Date: Jan 2014 Posts: 9 Rep Power: 5 dear mariam and sara, In fact FLUENT compute h (heat transfer coefficient) and NU number wrong and you should compute them manually as follows: h=mdat*cp*(Twall-Tbulk) Nu=hD/k Sincerely

 January 30, 2014, 08:59 #3 Senior Member   Join Date: Jan 2011 Posts: 272 Rep Power: 9 Hi Alek thanks a lot for the quick respond. You mentioned in your relation Twall & Tbulk? the problem I not have both of these temperatures because I used fixed heat flux at the wall not fixed wall temperature? So how I can predict Twall in this case?

 January 30, 2014, 09:23 #4 New Member   Smith Join Date: Jan 2014 Posts: 9 Rep Power: 5 The Twall which is computed with FLUENT is right and you can use it.

 January 30, 2014, 09:25 #5 Senior Member   Join Date: Jan 2011 Posts: 272 Rep Power: 9 Do you mean I need to plot Twall along the wall? what about Tbulk how i can compute it?

 January 30, 2014, 09:27 #6 New Member   Smith Join Date: Jan 2014 Posts: 9 Rep Power: 5 If you send me an email I can send you a good document.

January 30, 2014, 10:33
#7
Senior Member

François Grégoire
Join Date: Jan 2010
Posts: 389
Rep Power: 10
Quote:
 Originally Posted by Alek dear mariam and sara, In fact FLUENT compute h (heat transfer coefficient) and NU number wrong and you should compute them manually as follows: h=mdat*cp*(Twall-Tbulk) Nu=hD/k Sincerely
Careful maria, the equation Alek gave you for h is wrong: It's not the equation for h, it's the equation for the heat transfer.

Fluent calculates the heat transfert coefficient (h) from various correlations depending on the physics. It's your homework to verify in the Theory Guide which correlation Fluent uses according to the physics of your model, then decide if you should modify it or not.

Last edited by macfly; January 30, 2014 at 12:00.

 January 30, 2014, 11:44 #8 Senior Member   Join Date: Jan 2011 Posts: 272 Rep Power: 9 Hi Macfly I not have problem with the theory. I tried solve problem with constant heat flux at a cylinder wall with laminar flow case it must give me Nu=4.36 but it give different value? I am not one of fluent designer to know how FLUENT predict Nu values you answer is vague to me?

January 30, 2014, 12:08
#9
Senior Member

François Grégoire
Join Date: Jan 2010
Posts: 389
Rep Power: 10
Quote:
 Originally Posted by mariam.sara Hi Macfly I not have problem with the theory. I tried solve problem with constant heat flux at a cylinder wall with laminar flow case it must give me Nu=4.36 but it give different value? I am not one of fluent designer to know how FLUENT predict Nu values you answer is vague to me?
You don't have problem with the theory but it seemed like you bought what Alek said.

- maybe your mesh is not fine enough?
- maybe the flow is not fully developped?

What I'm saying wouldn't sound vague if you took a look at the theory guide in order to understand what Fluent is doing. I guess you're doing some engineering homework and you have to put some thinking into it. You don't become an engineer just clicking on buttons expecting to get the right number on the output.

 January 30, 2014, 12:19 #10 New Member   Smith Join Date: Jan 2014 Posts: 9 Rep Power: 5 Dear maryam and Sara you can use the following relations to compute h and NU manually: Q=q''Px=mdat*C*(Tbulk,x-Tbulk,in)->Tbulk,x=(q''Px/mdat*C)+Tbulk,in h(x)=q''/(Twall-Tbulk,x) Twall is calculated by Fluent macfly and mariam.sara like this.

 February 9, 2014, 02:12 How to make inlet velocity fixed along a pipe #11 Senior Member   Join Date: Jan 2011 Posts: 272 Rep Power: 9 Hello I have a query to how i can make the inlet velocity value fixed from pipe inlet until pipe outlet? is that possible in Fluent? knowing that the flow is laminar?

 July 28, 2015, 11:41 #12 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 998 Rep Power: 17 Question is not very clear to me; do you mean have a fully developed flow so to have a constant velocity profile? If so, just use periodic boundary condition. __________________ Google is your friend and the same for the search button!

July 29, 2015, 03:28
#13
Senior Member

Join Date: Jan 2011
Posts: 272
Rep Power: 9
Hi ghost if I want fully developed flow I can use periodic boundary by defining inlet as periodic boundary?? I need to know how to use periodic boundary??

mariam

Quote:
 Originally Posted by ghost82 Question is not very clear to me; do you mean have a fully developed flow so to have a constant velocity profile? If so, just use periodic boundary condition.

 July 29, 2015, 03:43 #14 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 998 Rep Power: 17 Yes, just change the inlet/outlet to periodic. Then in periodic settings set the pressure gradient or mass flow rate. __________________ Google is your friend and the same for the search button!

 July 29, 2015, 04:47 #15 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 998 Rep Power: 17 The main problem is how the heat transfer coefficient (h) is defined: as you know there is bulk temperature into the equation, but what is bulk temperature? Adjacent cell to the wall? Or temperature on the axis? Or....? For each defined bulk temperature you will obviously obtain different values of h, and so different values of Nusselt number. Related to your problem (fluid flow in pipe, laminar, with constant heat flux) I suggest to: 1- Draw 2D axisymmetric pipe 2- Set a periodic translational pipe 3- Enable energy equation, but disable in solution controls the energy equation (1 step: solve the momentum equation) 4- Once the velocity field is converged, eneable energy equation and disable momentum equation (2 step: solve the enrgy equation) 5- Create a line in y direction at a predefined x location (in the middle of the pipe for example) 6- Go to Reports->surface integrals->area weight average: select temperature and the line you created (This will be the mixed mean temperature, n other words Tbulk) 7- Evaluate the temperature on the wall, at the line you created 8- Calculate h as h=Q/(Twall-Tbulk), where Q is your heat flux (Watt/m2). 9- Evaluate Nusselt as Nu=h*D/k, where D is pipe diameter (m), k thermal conductivity (W/m/K) This should give you a good approximation. esinticik likes this. __________________ Google is your friend and the same for the search button!

 July 29, 2015, 05:04 #16 Senior Member   Join Date: Jan 2011 Posts: 272 Rep Power: 9 really thanks ghost82 for the valuable illustration. I will told you what I did, I run my case as described previously it converged and the contours of temperature is quite good when compared to the literature. I want now to predict h & Nu at a distance (0.69825 m) from the pipe inlet hence I draw a vertical line at this distance I evaluate Tbulk and used surface integral>area weighted average along the line Tb=298.6429 K then evaluated Tw at the wall which be 308.17706 K now I predict h from the relation knowing that heat flux at the wall is 8846.4 W/m^2 as below: h=8846.4/(Tw-Tb)=8846.4/(308.17706-298.6429)=927.8635978 W/m^2.K this value is higher than that predicted from experiments which is 888 W/m^2.K?? I can sent you my case file and the paper I compare with if you want have a look? Thanks mariam

 July 29, 2015, 05:09 #17 Senior Member   Join Date: Jan 2011 Posts: 272 Rep Power: 9 I forgot to mention my case not fully developed from inlet it a startup flow which be fully developed at the end pipe section only. So i think I do not need for periodic boundaries.

July 29, 2015, 05:12
#18
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 998
Rep Power: 17
Quote:
 Originally Posted by mariam.sara really thanks ghost82 for the valuable illustration. I will told you what I did, I run my case as described previously it converged and the contours of temperature is quite good when compared to the literature. I want now to predict h & Nu at a distance (0.69825 m) from the pipe inlet hence I draw a vertical line at this distance I evaluate Tbulk and used surface integral>area weighted average along the line Tb=298.6429 K then evaluated Tw at the wall which be 308.17706 K now I predict h from the relation knowing that heat flux at the wall is 8846.4 W/m^2 as below: h=8846.4/(Tw-Tb)=8846.4/(308.17706-298.6429)=927.8635978 W/m^2.K this value is higher than that predicted from experiments which is 888 W/m^2.K?? I can sent you my case file and the paper I compare with if you want have a look? Thanks mariam
EDit post: Sorry, I deleted what I wrote as it was wrong.

Send me the paper; I think that 927 vs. 888 should be acceptable, it's a 4% "error", I don't know..

Moreover: are you sure your simulation reflects 100% the experimental setup?

Daniele
__________________

Last edited by ghost82; July 29, 2015 at 15:24.

July 30, 2015, 11:04
#19
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 998
Rep Power: 17
Just to make public my thoughs I wrote you by email:
I think Tbulk could be calculated better by mass-weighted-average and not area-weighted-average.

Moreover,
Book "Fundamentals of heat and mass transfer" by Incropera defines a Tm (Tbulk), as in the attached picture.

I think you can create a custom field function named for example numerator:

density*axial-velocity*specific-heat-cp*temperature

Then evaluate the integral on the radial line you defined:
Reports->Surface integrals->Integral and choose Custom field function->numerator

Then divide this number by the (mass flow rate*cp).
Mass flow rate can be obtained in reports->fluxes.

If your cp is a function of temperature you can evaluate an average cp by mass-weighted-average.

Results of Tm should be similar to Tbulk evaluated by mass-weighted-average.

Daniele
Attached Images
 Tm.png (5.2 KB, 14 views)
__________________

November 23, 2015, 15:21
#20
New Member

Join Date: Mar 2009
Posts: 14
Rep Power: 10
Quote:
 Originally Posted by mariam.sara I forgot to mention my case not fully developed from inlet it a startup flow which be fully developed at the end pipe section only. So i think I do not need for periodic boundaries.
Hi Mariam,
I realize this thread is a bit old now, but can you explain further what you mean by the above statement? If your case is not fully developed it is not surprising that you would get a higher Nu than the theoretical result for fully-developed conditions. The temperature profile is flatter in the developing region, and the difference between the bulk temperature and the wall temperature is smaller than in the fully developed region. For a given fixed wall heat flux, this means h will be higher in the developing region. So it is important to use periodic conditions for temperature, not just velocity.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post flying OpenFOAM Running, Solving & CFD 28 December 30, 2013 16:05 danny123 OpenFOAM Running, Solving & CFD 4 June 19, 2013 04:49 samiam1000 SU2 3 March 25, 2013 05:55 marcoymarc CFX 33 March 13, 2013 07:39 danny123 OpenFOAM 19 October 24, 2012 07:44